using FCGear to cut a gear inside a gear
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using FCGear to cut a gear inside a gear
Hi All,
I'm having a difficult time cutting a gear inside a gear. I'm still learning FreeCAD and congrats to the multiple people who have worked on this over the years - pretty amazing value in this program.
The part I'm trying to recreate is an external Gear 1 (FCGear does a great job in creating it) that has a cutout in it where another gear gets pressed into it as a shaft - Gear 2. So Gear1 has a pocket for Gear 2.
FCGear has enough adjustment that i can dial in the gears to be about right - it's not a simple involute so I can create a representative gear for Gear 1 and also for Gear 2 but I cannot seem to either
a) Use Part WB to subtract 1 from the other
2) Use Part Design to turn Gear 2 into a sketch and then pocket Gear 1
3) Use Draft to create a 2D representation of Gear 2 and then use Part Design to create a pocket in Gear 1
Any simple way to do this?
Thanks in advance
enmane
I'm having a difficult time cutting a gear inside a gear. I'm still learning FreeCAD and congrats to the multiple people who have worked on this over the years - pretty amazing value in this program.
The part I'm trying to recreate is an external Gear 1 (FCGear does a great job in creating it) that has a cutout in it where another gear gets pressed into it as a shaft - Gear 2. So Gear1 has a pocket for Gear 2.
FCGear has enough adjustment that i can dial in the gears to be about right - it's not a simple involute so I can create a representative gear for Gear 1 and also for Gear 2 but I cannot seem to either
a) Use Part WB to subtract 1 from the other
2) Use Part Design to turn Gear 2 into a sketch and then pocket Gear 1
3) Use Draft to create a 2D representation of Gear 2 and then use Part Design to create a pocket in Gear 1
Any simple way to do this?
Thanks in advance
enmane
Re: using FCGear to cut a gear inside a gear
Hi and welcome to the forum!
Your proposal a) should work. Upload your file for more help.
Your proposal a) should work. Upload your file for more help.
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Re: using FCGear to cut a gear inside a gear
I started with just simple spur gears and it seems to work fine by just creating both gears and then pocket the second within the first. As soon as I add details of the gears, it seems to break...
FreeCad 0.19 - latest download as of 1/10/2022
Gear 1 -
Teeth 27
Mod - 1.1
Beta = -25
clearance = 0.2
Gear 2
Teeth 6
Mod 1.5
Clearance = -.5
Tip 0.2
Also - add that Gear 2 should be scaled by 1.05% as well for clearance.
FINALLY got something to work but not sure how to scale and VERY temperamental - system hangs and crashes...
File added...
FreeCad 0.19 - latest download as of 1/10/2022
Gear 1 -
Teeth 27
Mod - 1.1
Beta = -25
clearance = 0.2
Gear 2
Teeth 6
Mod 1.5
Clearance = -.5
Tip 0.2
Also - add that Gear 2 should be scaled by 1.05% as well for clearance.
FINALLY got something to work but not sure how to scale and VERY temperamental - system hangs and crashes...
File added...
- Attachments
-
- gearfile.FCStd
- (837.53 KiB) Downloaded 21 times
Re: using FCGear to cut a gear inside a gear
Almost there....
If I can scale Gear 2 1.05% then I'm done..
For those of you interested in what this is - it's a gear for a paper shredder - the one that usually strips when an Aunt puts too much paper in
I tried uploading the one that is currently working without the scaling but file size is too large at 1.53MB
If I can scale Gear 2 1.05% then I'm done..
For those of you interested in what this is - it's a gear for a paper shredder - the one that usually strips when an Aunt puts too much paper in
I tried uploading the one that is currently working without the scaling but file size is too large at 1.53MB
Re: using FCGear to cut a gear inside a gear
Using Pat Wb you could also scale it, once create is a solid and could be modified with all the usual solid methods, and commands.
Regards
Carlo D.
Regards
Carlo D.
GitHub page: https://github.com/onekk/freecad-doc.
- In deep articles on FreeCAD.
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- In deep articles on FreeCAD.
- Learning how to model with scripting.
- Various other stuffs.
Blog: https://okkmkblog.wordpress.com/
Re: using FCGear to cut a gear inside a gear
Hello enmane, greetings to the Community!
I saw your file, the difference boolean function, you can do it with "Part" (as @chrisb already advised you) not with "Part Design" (this is what causes the error) as you have two solids (gears already modeled) distinct.
I have read the data relating to the helical toothing, I ask you: - does the module (1,1) you entered refer to the normal module or to the transverse one?
I am attaching your revised file only in the procedure concerning obtaining the central pocket by applying method a) (stated by you and not applied)
I hope you are familiar with the gears (I mean in the sizing), here something can come in handy https://forum.freecadweb.org/viewtopic. ... 88#p558688.
Before printing (to avoid unpleasant surprises), I advise you to check the dimensions (normal pitch, cross pitch, helix inclination, helix direction, external diameter, internal diameter, tooth thickness, tooth height, etc.) to check if they interface correctly on the gears with which it must mate.
This advice must also apply to the internal "gear" used to obtain the pocket.
- Attachments
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- gearfile.FCStd
- (400.18 KiB) Downloaded 13 times
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- gear_cut.png (147.64 KiB) Viewed 1384 times
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- Veteran
- Posts: 5505
- Joined: Thu Apr 05, 2018 1:53 am
Re: using FCGear to cut a gear inside a gear
If it's a press fit you might not want much clearance.
Re: using FCGear to cut a gear inside a gear
Thanks all
-I'm very familiar with gearing and have printed both of the gears individually and they are geometrically correct. If you take a paper shredder apart you'll see the shaft of the shredder motor - 1st gear is more like 3 rods of steel welded together and twisted into a helix...very non-standard but I confirmed the dimensions through measuring and printing and ensuring mesh...
I will try to see how this works through Parts WB...
Thanks in advance...
Domad,
I noticed that you did not create a Part or Body. What don't I understand about FreeCAD that it was so obvious for you? It seemed as soon as I moved those parts out of the Body and out of the Part then it worked fine. Where do I read to get up to speed on recommendations between types of parts/bodies/entities and which workbenches work with them? Note: I have done A LOT of reading over the past 3 weeks and it still isn't clear.
Can I ask that you scale the center object as I go to Draft WB, create a clone, then click on the clone and change the scale from 1.0 to 1.05 and it doesn't take - it reverts back to 1
-I'm very familiar with gearing and have printed both of the gears individually and they are geometrically correct. If you take a paper shredder apart you'll see the shaft of the shredder motor - 1st gear is more like 3 rods of steel welded together and twisted into a helix...very non-standard but I confirmed the dimensions through measuring and printing and ensuring mesh...
I will try to see how this works through Parts WB...
Thanks in advance...
Domad,
I noticed that you did not create a Part or Body. What don't I understand about FreeCAD that it was so obvious for you? It seemed as soon as I moved those parts out of the Body and out of the Part then it worked fine. Where do I read to get up to speed on recommendations between types of parts/bodies/entities and which workbenches work with them? Note: I have done A LOT of reading over the past 3 weeks and it still isn't clear.
Can I ask that you scale the center object as I go to Draft WB, create a clone, then click on the clone and change the scale from 1.0 to 1.05 and it doesn't take - it reverts back to 1
-
- Veteran
- Posts: 5505
- Joined: Thu Apr 05, 2018 1:53 am
Re: using FCGear to cut a gear inside a gear
Consider the PDWrapper macro.
Here you would wrap the inner gear as a subtractive feature and scale it at 1.05.
1: remove pocket
2: remove involutegear001 from the body. (Edit the body's Group property to no longer include this object.)
3: tell involutegear001 it no longer has a BaseFeature. (select involutegear001, Ctrl+Shift+P, in the python console enter
4: wrap involutegear001 as a subtractive feature using PDWrapper macro. (install PDWrapper, run once to create .py file it needs, select involutegear001, run macro, select subtractive as the type, tell it to follow involutegear in the tree, later toggle claim children property to true)
5: scale involutegear001. (select pdw_sub object, in the property view at bottom toggle show scale props to true, set tip tool scale to 1.05.)
Here you would wrap the inner gear as a subtractive feature and scale it at 1.05.
1: remove pocket
2: remove involutegear001 from the body. (Edit the body's Group property to no longer include this object.)
3: tell involutegear001 it no longer has a BaseFeature. (select involutegear001, Ctrl+Shift+P, in the python console enter
Code: Select all
obj.BaseFeature = None
5: scale involutegear001. (select pdw_sub object, in the property view at bottom toggle show scale props to true, set tip tool scale to 1.05.)
- Attachments
-
- gearfile_markster.FCStd
- (585.43 KiB) Downloaded 14 times
-
- Veteran
- Posts: 5505
- Joined: Thu Apr 05, 2018 1:53 am
Re: using FCGear to cut a gear inside a gear
Alternatively, use WireFilter to offset a SubShapeBinder of the face and pocket the WireFilter. For this you need to install the WireFilter macro.
1) Delete pocket.
2) Select face used to create pocket and create green SubShapeBinder.
3) Select SubShapeBinder and run WireFilter macro.
4) Set WireFilter Offset property to desired offset. Here I used 0.2 mm:
5) Select WireFilter, make pocket. Note: I had to delete Pocket to make the file small enough for the forum.
1) Delete pocket.
2) Select face used to create pocket and create green SubShapeBinder.
3) Select SubShapeBinder and run WireFilter macro.
4) Set WireFilter Offset property to desired offset. Here I used 0.2 mm:
5) Select WireFilter, make pocket. Note: I had to delete Pocket to make the file small enough for the forum.
- Attachments
-
- gearfile_markster2.FCStd
- (655.75 KiB) Downloaded 22 times